Components Panel

The Components panel provides direct access to available Workspace components, and database and file-based library components in Altium Designer.

The panel sources components from a connected Workspace and any open or installed libraries. The panel offers full details of the selected component (Parameters, Models, Part Choices, Supplier data, etc.), component comparison, and for Workspace components, a filter-based parametric search capability for specifying target component parameters.

The Components panel uses the basic search engine functionality and view that is applied in the Manufacturer Part Search panel. While the Manufacturer Part Search panel harnesses the Altium Parts Provider service and focuses on the component manufacturer and supplier data searches, the Components panel is populated with ready-to-place components from your connected Workspace and database and file-based library sources.

Panel Access

To open the Components panel, select View » Panels » Components from the main menus or the Components option from the button menu at the lower right of the main screen. Using a responsive design configuration, the panel layout will dynamically adapt between full-screen normal mode () and its compact mode () where the Categories/Filters options collapse to menus.

From within a schematic document, use the P, P keyboard shortcut to open the Components panel. From within a PCB document, use the P, C keyboard shortcut.

The Components panel in its normal mode. Hover the cursor over the image to see the panel in compact mode.

The panel’s Categories pane (or the drop-down menu in compact mode) lists all available Workspace components under the All category entry and any available libraries. When the panel is in its normal mode, click the Categories list icon or the « icon to collapse or expand the display of the column and use the button (top right) to toggle the visibility of the component Details pane. When sifting through the Categories pane, the Up/Down and PgUp/PgDn keyboard shortcuts may be used to walk through the list. The Left/Right keyboard shortcuts may be used to open and close the individual branches.

Libraries Menu

The operations menu options provide you the ability to set file-based libraries preferences, perform searches, and specify if component models collection is visible. To access these options, select the operations menu button at the top right of the panel.

File-based Libraries Preferences

Select the File-based Libraries Preferences command from the menu to open the Available File-based Libraries dialog, where you may view controls to add or remove libraries, install libraries, and specify library search paths. The Available File-based Libraries dialog has three tabs and is described in the following sections.

Project Tab

This tab lists all of the libraries that are part of the active project (the project currently selected in the Projects panel).

To add a library to the project, click the Add Library button. A dialog will open in which you can browse to and select a library file that you want to add to the project.

The following types of library files are supported as project libraries:

• Integrated Libraries (*.IntLib)
• Schematic Libraries (*.SchLib)
• Database Libraries (*.DbLib)
• Footprint Libraries (*.PcbLib) – only viewable if the Footprints option is enabled from within the Libraries menu.
• PCB3D Model Libraries (*.PCB3DLib)
• Sim Model Files (*.Mdl)
• Sim Subcircuit Files (*.Ckt)
• SIMetrix Model Libraries (*.LB)
• Ibis Model File (*.IBS)

Use the Move Up and Move Down buttons to define the search order of the libraries.

Installed Tab

This tab lists all of the installed libraries. This list is an environment setting. Any libraries added to the list will be available for all projects and the list is persistent across design sessions. Project libraries can be added to this list but are not initially part of it.

Click the Install button then select Install from file to open a dialog in which you can select the desired library you want to add to the list.

The following types of library files are supported as installed libraries:

• Integrated Libraries (*.IntLib)
• Schematic Libraries (*.SchLib)
• Footprint Libraries (*.PcbLib)

Use the Move Up and Move Down buttons to define the search order of the libraries.

Search Path Tab

This tab lists all libraries that have been found along the Library Search Paths for the project. These paths are defined in the Search Paths tab of the Project Options dialog. Click the Paths button to open the Search Paths tab to define further search paths or modify existing ones as required.

Use the Refresh List button to update the search paths and ensure that the library list is current.

Libraries in this tab are searched in the order they appear. Click the Paths button to define the order. Search paths can be defined as a specific file or to a folder, including subfolders.

File-based Libraries Search

When you do not know which file-based library contains a component or if it is even available, you can search for it. To search for a component, select the File-based Library Search option from the libraries menu () at the top of the panel to open the File-based Libraries Search dialog.

The searching process can be summarized as follows:

• Searching is performed by defining Filters that are applied to all libraries that can be searched according to the current search Scope settings.
• The Scope includes the type of libraries to search. Only one type can be searched at a time.
• The Scope defines which libraries will be searched: either the libraries the software currently has access to (Available libraries) or all libraries within a folder (Libraries on path).
• When searching libraries on a path, the target is a specific folder and can also Include Subdirectories.
• You also can search within the search results by setting the Scope to Refine last search.

Setting the Search Filter

The Filters region is used to define text strings that are to be applied to searching. There are three regions to configure:

• Field – this is the attribute of the component that is to be searched. It can be any component or footprint attribute including the Name, Description, Comment, Footprint, or any parameter that has been added to a component.
• Operator – defines how a match is determined. This can be when the value equals, contains, starts with, or ends with. Note that equals require an exact string match so it should only be used when you are confident that the search string is correct and complete.
• Value – the characters to be searched for in the chosen Field matched according to the chosen Operator.

Setting the Scope

There are essentially two approaches to searching:

• Libraries currently available – this is the list of libraries shown in the drop-down at the top of the Components panel.
• Libraries stored in a specific folder along with subdirectories if the option is enabled.

Searching will return all items of the chosen search type (Components/Footprints/PCB3D Models) found in all libraries that fall under the defined Scope (Available Libraries/Libraries on path on the specified search path). For example, if you want to find a component that you think is in a library within specific folders on the hard disk and that library was not currently listed in the Available File-based Libraries, you would define the search as follows:

1. In the Scope region, set Search in to Components and select Libraries on path.
2. In the Path region, set the Path to point to the folder containing the library document that you want to search.
3. Click Search.

Models View

Select the Models option in the panel's upper libraries menu () in order to include library model collection entries in the Categories listing. The additional entries in this browsing mode include Symbol, Footprint and Simulation model collections sourced from the connected Workspace, and also installed PCB footprint libraries (*.PcbLib).

In the Available File-based Libraries dialog, Footprint Library files will be listed under the dialog's Project and Installed tab regardless of the Models view setting.

Components List

Within the component listing grid itself, the content that is included in the list is managed by:

• Setting the component listing sort order – click a column heading to sort the component listing by that column data. Click the heading again to reverse the sort order.
• Setting the order of the displayed columns – drag and drop a column heading to a new position.
• Specifying which parameter columns are shown – right-click in a column header and choose Select Columns to open the Select Columns dialog then toggle a parameter column’s visibility and move its positional order with the Up/Down buttons.

• Grouping the list by column data – right-click in a column header, select the Enable Columns Grouping option then drag a column header (e.g., Footprint) into the grouping space at the top of the list. The list entries will be collected under each unique parameter (e.g., type of footprint) from the specified grouping column.

  When using Grouping to collate components in the listing, there is a limit of 10,000 entries that can be accommodated.
• Filtering the listing by a specific column entry – select in a column header to display a list of its unique parameter entries then select an entry to constrain the listed components to those that include the specified parameter (e.g., a footprint type code). Select the All option to reset the filter. Select (Custom) to open the Filter Editor dialog in order to further refine the filtering in the selected column.

Displaying Columns

There are various manners in which you may display the contents within the Components panel. When right-clicking on the names of each column (Name, Description, Footprint) you may select from the following options, depending on how you wish to display the components:

• Best Fit – merges the contents from the Name and Descriptions columns together so they are closely placed, with no excess room between each column.
• Best Fit All Columns – merges the contents from all columns together so they are closely placed, with no excess room between each column.
• Clear Sorting – used to undo the sorting of columns.
• Enable Columns Grouping – allows you to drag column headers by a specific column, allowing you to change the order of the Name, Description, and Footprint columns.
• Select Columns – opens the Select Columns dialog, which allows you to select other columns you would like visible in this section.
• Apply Column Visibility to Child Categories – in cases when the selected category has a child category, use this command to ensure the possibility of pushing column visibility settings from parent categories to child categories. This command is available only when a child category exists.

Component Search and Functions

Searching for components

To search for available components in the Components panel, enter a phrase in the Search field and/or use the panel's Categories and Filters selections to narrow the component listing to your specific needs. Filters are supported for Workspace components only, and as in the Manufacturer Part Search panel, the Components panel supports unit-aware (text to number) search filters. The search functionality prioritizes results according to the entered search criteria.

The Search function allows you to select then edit or add to an active Search string. Click the 'active' search string to enter it into the Search field. You can reuse or edit that search from the Search field.

The Find Similar Components dialog provides the possibility to define search preferences based on the selected component.

The Find Similar Components dialog is used to define your search preferences based on the selected component. The final search results will depend on the selected component type, be it Workspace or non-Workspace components, and your Workspace connection status. For example, Workspace components will often display more parameters than a non-Workspace component. To specifically gather components and parameters that are the same or different from the one selected, the drop-downs may be utilized to select Same, Any, or Different choices.

The dialog can be accessed by right-clicking on a listed component, then selecting Find Similar Components.

Placing Components

A selected component is placed on a schematic by dragging and dropping, by selecting Place from its right-click context menu, by using the button in the Details pane, or by using the Enter hotkey.

Filtering Through Components

When viewing Workspace components, the Filters pane is populated by selected filter options based on the current search and available parameters. Parametric filtering of the listed components provides further options for locating a specific component or type of component. Open the Filters pane from the button above the Categories pane.

Note that filters are only supported for Workspace components. Use the Filter Search field within the pane to find a specific parameter filter, and in the panel's narrow/docked mode, click the button to pop out the Filters as a panel extension.

The panel Filters options can be tailored to your needs by selecting particular parameter types as Favorites, which then shift to the top of the list for the current component Category. Hover to the right of a parameter filter’s name and click the icon to set the filter as a Favorite. Favorite filter settings apply to and are saved for individual component Categories.

To reset your favorites to the five default parameters, right-click then choose Reset Favorite Parameters.

For Workspace components, the right-click menu offers options to edit the component through the Single Component Editor (Edit) and perform component management functions such as component creation and cloning, or editing the selected component's Part Choices and Type (Operations).

Additional information options in the component Details pane include: viewing a model image, viewing online datasheets (References), live Supplier information (Part Choices), seeing where the part has been used in Workspace projects and Managed Sheets (Where Used), and through the right-click menu, the ability to copy selected or all component parameter data (technical details) in a tab-delimited format, and resetting favorites.

When browsing the components in a connected Altium 365 Workspace and if any issues regarding the health of the selected component are found, an indication of it will be presented by the  (for errors) or  (for fatal errors) icon in the Component issues line above the component parameter list. The number at the right of the icon indicates the number of found issues. Click the down arrow at the right of the number to see the short descriptions of the issues.

An example of library health issues found.

You may use the custom filtering feature to further refine filtering in the Components panel. The feature is available by clicking the filter () icon in the header, then selecting (Custom). This will open the Filter Editor dialog, which allows you to define the condition, operator, value, operator type, etc., for which you want to filter results.

Where Used

The Where Used drop-down tracks where a particular component is located. You may select the Project, Managed Sheets, or All buttons to view the particular project, managed sheet, or both, in which the given component has been used. Information regarding the date and time of placement is available, as well as information regarding the soft delete feature, in the case that the component has been deleted.

Operating as a 'soft delete', the removal process provides increased options and information as you proceed, including relevant links to source items for review purposes. Items can be deleted by users who have editing rights to those items and can be restored from within the Workspace's browser interface. In the Workspace, deleted items are moved to a dedicated Trash location where they can be retrieved (Restore) by users who have editing rights to the deleted items, or completely removed (Permanently Delete) by Workspace administrators or the owner of those items.

Component Data Caching

When using the Components panel, the data for Workspace components are cached to the local machine from the Workspace. This provides an offline access mode for Workspace components when Altium Designer is not connected to the Workspace, and therefore allows normal component browsing and placement, etc. Note that Filters are not enabled in this mode.

This condition is indicated by the 'Offline mode – cached data is being used' warning text in the lower bar of the panel’s component list pane. The cache builds up component data over time and may be cleared (for all Workspaces) using the Clear Cache option that is available under Known Servers in the Data Management – Servers page of the Preferences dialog.

Part Choices List

Edit the Part Choices List associated with a Workspace component by selecting the Operations » Create/Edit PCL option from the entry’s right-click menu.

Use the following Edit Part Choices dialog’s button to open the Add Part Choices dialog, which will automatically search for part manufacturers by the selected component's Name parameter. Deselect the predefined search term to manually search for alternatives – functionally, the dialog is a modal version of the Manufacturer Part Search panel.

Part Choice entries in the list can be ranked by selecting an appropriate star icon level, where the list will automatically be reordered with the highest-ranked manufacturer choice at the top.

A Part Choices List is carried with the component wherever its data is applied, such as in a Schematic design, BOM document, Output Report, and so on.

Right-click Menu

The right-click pop-up menu for the panel provides the following commands:

• Place [ComponentName/FootprintName/SimulationModelName] – use to place the currently selected component or simulation model onto the active schematic document or currently selected footprint onto the active PCB document.
• Find Similar Components – use to open the Find Similar Components dialog to set up search criteria to find components similar to the selected component.
• Edit – click to edit the selected Workspace component through the Single Component Editor or selected domain model (symbol, footprint, or simulation model) in its editor. For a component, if the current component type is different from the template that is currently being used, the Change component type dialog will open. Use the dialog to change the component type of the selected component.
• Navigate to [ComponentName] – use to open the chosen Workspace component in the Explorer panel, where you may access detailed Item information and manage the revision and lifecycle settings for the Items well as where-used and supply chain detail, amongst other options.
• Operations – use to access a drop-down menu of additional functions for Workspace components as described below.
  • Submit Request – this option is accessible only when using Altium NEXUS.
    Submit Request – use to access the active part request process definitions. If no active process definitions are available for the Part Requests process theme, the Submit Request button will be grayed out (not available). You may need to sign out of the Workspace and back in again or restart Altium NEXUS to refresh.
  • Create – click to open the Create new component dialog to select the type of component when adding a new component.
  • Download – click to download the selected component(s) to a zipped Integrated Library Package.
  • Clone – click to clone (copy) the selected component. The component editor opens in the Single Component Editor mode.
  • Delete – click to delete the selected component(s) from your connected Workspace.
  • Change Component Type – use to open the Choose component type dialog, where you may alter the component's type, add a subtype, or merge component types, amongst other options.
  • Change State – use to change the revision state of the selected component(s). After using the command, the Batch state change dialog opens, which allows you to change the revision state of the component(s).
  • Create/Edit PCL – use to access the Edit Part Choices dialog, where you may create or edit the part choices list associated with the Workspace component.
  • Full Item History – use to access a detailed view for the currently selected component, opened as a new tabbed view within Altium Designer. The Item View provides a highly detailed view of the Revision and Lifecycle history of a specific Item, as well as showing all of the elements that make up that Item. The view also includes a Timeline. Use the Timeline to examine the exact time and date of any change made to the Revision level or Lifecycle State of that Item and who made the change.
• Refresh – click to quickly refresh the panel. The current component selection will be saved

Compare Feature

The Compare feature allows you to compare the parameters of two selected components (parts). This feature is accessed by selecting two components in the grid region with the icon enabled (blue). The Selected Component Details region opens to the right of the grid region. The upper region (region 1 in the image below) displays an image, the name, description, and price of the selected components side-by-side. Click the Datasheet button to open the manufacturer's datasheet (if available) for the associated component. Click the Place button to place the component in the design space. The component will appear floating in the design space; click to place the component in the desired location. You can continue to place additional components or right-click or Esc to leave placement mode and return to the Components panel.

The lower region (region 2 in the image below) displays a side-by-side view of the components' parameters, with differences highlighted in red text for easy comparison.

The Compare feature is also available when the Components panel is in compact mode, though works a tad differently. This feature is accessed by selecting two components in the grid region. The Selected Component Details region opens below the grid region. The upper region displays the name, price, and view of the components' parameters, with differences highlighted in red text for easy comparison. The lower region displays a side-by-side view of the components' Symbols and Models.

Editing Component Symbols and Footprints

The symbol and footprint of a given component can be hidden within the Models section of the Details pane, which is accessed by clicking on the upper right. Once hidden, the symbol and footprint will be replaced with clickable links that revert the hidden items to their original view. Also included is the ability to scale the size of the displayed models. For both the symbols and footprints, click and drag the lower perimeter of the model area to resize the image.

For a Schematic Library (.SchLib) file being browsed in the Components panel, the symbol and footprint of the selected component can be edited using the  button at the bottom-right of the model preview.

The ability to edit a footprint is made available when accessing the Components, as long as valid and linked footprints are already present.

Component Selection Dialogs

The search engine and view used in the Components panel is also applied in other Altium Designer applications where a component choice is made. The component search functionality is included in these (modal) dialogs, along with an OK confirmation button and minor variations in the available action commands. The dialog is typically called Component Search.

• ActiveBOM document – the Components search view is used when changing a Workspace component to an alternative component. Right-click on a listed component item and select Change [component name] from the context menu to open the Replace Component dialog.
• Item Manager – the Components search view is used when manually choosing a Workspace component to replace the current component. Right-click on a listed component item and select Choose manually from the context menu to open the Replace Component dialog.
• Variant Management – the Components search view is used when choosing an alternate component project variation. Select an Alternate part as a Component Variation, then Choose in the Edit Component Variation dialog to open the Replace Component dialog.